1
\$\begingroup\$

I bought this three phase rectifier from local store and it has rectangular connectors, enter image description here

Now I need to make its package on the ARES, but I cant figure out how to create rectangular holes in the package.

\$\endgroup\$
  • 5
    \$\begingroup\$ The much harder question is where to get the rectangular drill bits from. \$\endgroup\$ – Olin Lathrop Jul 21 '14 at 16:36
  • \$\begingroup\$ Ie, you need to find out if your fab supports milling slots (and if so, what minimum width and if they will end up plated), if they will tolerate overlapping drills, etc. Then you can figure out how to specify that in your software. \$\endgroup\$ – Chris Stratton Jul 21 '14 at 16:37
  • 1
    \$\begingroup\$ Then your question should really be, "what do I want the toner to do that will make my fabrication life easier" and figure out how to draw that. I'd consider things like two small holes in a larger copper pour, or just a single hole and plan to get a needle file in there. Actually for a one-off prototype I'd probably surface mount it on the solder side as I hate drilling holes. \$\endgroup\$ – Chris Stratton Jul 21 '14 at 16:48
  • 4
    \$\begingroup\$ That package is not intended to be mounted on a PC board - it would normally be bolted to a heatsink or chassis, and connected to the PC board with wires, terminated in female spade (Faston(tm)) connectors that would be pushed onto the terminals, or the wires could be soldered to the terminals. \$\endgroup\$ – Peter Bennett Jul 21 '14 at 17:04
  • 3
    \$\begingroup\$ see electronics.stackexchange.com/questions/66102/… for a previous discussion on a similar package - with pictures. \$\endgroup\$ – Peter Bennett Jul 21 '14 at 17:45
1
\$\begingroup\$

To answer the actual question: "How do I create rectangular holes?":

In the PCB programs I've used (mostly Protel/Altium) there is no built-in way to specify rectangular holes,as few board shops have rectangular drills.

If you want non-round holes or other special milling on a board, you will have to discuss the matter with the board shop to determine if they can do what you want, and how they want it specified. (I've seen suggestions to mark the ends of a slot with a non-drillable hole size (perhaps .001"), so the board shop will have to consult you or a readme file to find out what you really want.)

Since you will be making this board yourself, using home-brew techniques, you just have to produce artwork that you will understand.

\$\endgroup\$
6
\$\begingroup\$

Forget rectangular holes!

This kind of part is usually bolted to a heat sink, "dead bug style" (legs pointing into the air). The terminals do not go through a PCB; it is not a through hole part.

The terminals accept sliding "push on terminal" connectors.

enter image description here (source of picture)

\$\endgroup\$
  • \$\begingroup\$ I agree with your point that O.P.'s rectifier was intended for off-board mounting. At the same time, your post is more of a comment than an answer. The answer to the question "How to specify plated slots?" is applicable to other components, which are intended to be board mounted. \$\endgroup\$ – Nick Alexeev Oct 11 '14 at 23:51
2
\$\begingroup\$

To create a SLOT in ARES(PCB part of Proteus) requires 3 things. First is the ability of your PCB Fabricator to route out slots, and to know his minimum routing tool size. The jokes about rectangular drills are not very funny for someone asking for help.

Second, [C]reate a "PAD" in DILPAD mode. Make a name [ie SLT-100x40DP], then click OK. Next window you make the PAD dimension the outside dimensions of the copper for your slot. The drill hole should be .005" greater than the preferred or minimum routing tool of your PCB fabber. Smallest I see looking around is 0.5mm - .020", but you have to find out

Third, [C]reate a "PAD" in PADSTACK mode. Make a name, different than your DILPAD name [ie SLT-100x40], then select the DILPAD you created [ie SLT-100x40DP] in the Initial Style drop down box Under STYLE NAME select SLOTTED. In the SLOT box enter your slot dimensions [w=20th h=100th] and your PCB Fabber's slotting tool dimension[t=0.5mm]. Allow for copper plating thickness and round corners in deciding to the dimensions of your slot. On the right you can see what other layers you may wish to connect to, if you never do multi-layer boards, this info doesn't matter. You can always edit this later.

Click OK. iIn the list of available PAD STACKS your new plated slot [ie SLT-100x40] is available to use like any other hole or pad making a new package. Edit as needed. Finished slot info is placed on the Mechanical layer so be sure to include this layer in your Gerber .zip

Slots are handy, specially in high frequency applications- such as for a PCB mount antenna connector. Besides saving board space, solder has more capacitance than copper. A big hole could cause your project to function poorly. A ton of solder in a big hole is not an ideal solution.

However, that said above, slots do cost more than holes, and lots of the less expensive PCB proto places won't allow slots. So, find out the cost of a slot vs. a hole in your application, then make your choice.

\$\endgroup\$

Your Answer

By clicking “Post Your Answer”, you agree to our terms of service, privacy policy and cookie policy

Not the answer you're looking for? Browse other questions tagged or ask your own question.